Drill Posting

[Robert Barton]

I am trying to post a drill program in 9.1 SP2 and I’m having a problem.

 

In the drill operation I would like to use the Ref point, in the Tool Parameters and set an Approach of 1”, then on the second drill tab I would like to set the Clearance at .5” and then just below that I would like to set the Retract height to .1” hoping to post out a program like below:

 

G43 H1 Z1. M8

Z.5

G99 G81 Z-.6 R.1 F10.

X2.625 Y.9375

G80

 

But I only get this:

 

G43 H1 Z1. M8

Z.1

G99 G81 Z-.6 R.1 F10.

X2.625 Y.9375

G80

 

It seems to skip the Clearance height altogether.

 

The reason I would like to do this update is because we always want any tool to start at 1” above the part, then I would like to have better control of my drill cycles most notably when I use a Neg. R value

 

I cannot seem to post something like this out:

(note the G99 has changed)

 

G43 H1 Z1. M8

Z.5

G98 G81 Z-.6 R-.1 F10.

X2.625 Y.9375

G80

 

I have tried to change the post but so far I’ve been unsuccessful, any help would be greatly appreciated.

I use a HAAS post but no post seems to help me.

 

Thanks

[Guest]

Robert, I don't know that what you want to do is possible short of hard coding it into the post or setting up another variable that you would have to enter into every drill cycle.

 

 

As you can see your Clearance height is controlled as is your retract height but there is not another place to enter a value as you are seeking.

 

What you are looking to do is really not necessary anyways. You can already keep your drill down at the G99 plane or a full clearance to a number of your choice, is it really necessary to add another value in there?

 

What's the purpose of the in-between numbers?

[crazy^millman]

Can you use Ref point on the operation page to accomplish this?

[Robert Barton]

The reason for these in-between numbers is because we want to start our tools at 1” above and then turn the coolant on, also it’s so we can rapid down to say R-.25 and yet jump up to +.1 (G98), for the next hole, without jumping all the way back up to the 1” where we turned the coolant on.

 

To post out a program like this:

 

G43 H1 Z1. M8

Z.1

G98 G81 Z-.6 R-.25 F10.

X2.625 Y.9375

G80

 

Jumping up to 1” is not so bad but if the Ref point is say 12” as for on a horizontal milling machine, I do not want to jump back up to 12” between every hole. In this case I could set the retract to +.1 and check the box for a G99, but I would have to start drilling from the +.1, rather than from the -.25 In this example I want to jump up to +.1 before moving to the next hole so I can jump over bosses or islands, but I am drilling into the bottom of a pocket.

 

Maybe I could edit the geometry and edit the jump heights to accomplish this, but I haven’t tried this yet.

 

Using the Ref point on the first page seems to cancel out the Clearance plan on the second page.

 

Thanks for you're help so far.

[Guest]

Jump heights is probably the best way for you to accomplish this.

 

I tried Ron's suggestion on the ref height and it works to a point but there is the added step of making sure the ref postion start and end coincides with your start and end holes.

 

 

Now as far as the reasons why, this really is a pointless endeavour, with the rapids available on todays machines the difference between an 1", 2" or evan a 4" rapid is ultimately nothing. This sounds like something that someone wants done becasue this is the way we've always done it kind of thing.

 

The time savings, your boss I assume, thinks he is saving by doing it this way don't exist. You could run it full retract and in the end you time will be darn lose to the same. So unless your machining 20,000 pcs there is nothing to be gained in doing it this way. You'll save more time on the programming end using the code as it is created and NOT having to worry about adding in some extra movement.

 

JMO

 

[Rakesh]

may he should use manual entry option to put z1. and just copy after the operations

[dwsz71]

/// deleted ///

[Roger Martin from CNC Software]

What HAAS post are you using?

From the install or a version of the MP-MASTER ?

 

From what I see, what you’re looking for is possible using the std. parameters available.

 

You have these settings to work with:

The Approach Reference Point (Z axis only) of 2.0

The Clearance of 1.875

The Retract is 0.125

The Depth is -0.5

= 4 ‘Z’ values available in the NCI data going to the Post Processor.

 

The bolded value below is the Initial Height (which I added the the PST to get this output).

The Post variable name for it is = initht

If Clearance is ON, initht is loaded with the Clearance value.

If Clearance is OFF, initht is loaded with the Retract value.

 

G0 G90 G54 X-3. Y1.5 A0. S1000 M3

G43 H1 Z2. M8

Z1.875

G98 G81 Z-.5 R.125 F8.45

X-2.125 Y.875

X-.2525 Y-.375

G80

 

So…

With some logic added to the PST, you could handle these multiple ‘Z’ scenarios.

[Tim Johnson]

Also check the "Use clearance only at the start and end of operation" check box for G99 and uncheck the box for G98.

[Robert Barton]

This is the post that I’m using:

 

# Post Name : MPFAN

# Product : MILL

# Machine Name : GENERIC FANUC

# Control Name : GENERIC FANUC

# Description : GENERIC FANUC MILL POST

# Associated Post : NONE

# Mill/Turn : NO

# 4-axis/Axis subs. : YES

# 5-axis : NO

# Subprograms : YES

# Executable : MP 9.0

 

I’m using 9.1 SP2

 

I’ve modified this post a lot now since we first started using it, including Custom drill cycles. Now I use it as a post for our Makino Horizontal milling machine, it was and is still used as our Vertical Milling machine post as well, of course with some changes.

 

I figured out that the variable that I need is initht, but I’m having a hard time figuring out where, exactly, to put the variable to post out the value where you have it listed below (Z1.875) This is exactly what I’m looking for.

 

I’ve tried putting initht in pdrill0, pdrlcommonb, prdrlout (it doesn’t belong there) and pdrill. No point in putting it in any of the other Canned Drill Cycles, I can test it in pdrill. But I haven’t had any luck getting exactly what you have listed below.

I got it to post the initht value right after the “G80” once or twice though, but I can’t get even that now.

 

I guess I’m just not sure how the logic flows in the post, or maybe I’m just out of logic altogether.

 

Please help me, please tell me where to put initht.

 

Thanks for any help you may be able to give.

 

 

What HAAS post are you using?

From the install or a version of the MP-MASTER ?

 

From what I see, what you’re looking for is possible using the std. parameters available.

 

You have these settings to work with:

The Approach Reference Point (Z axis only) of 2.0

The Clearance of 1.875

The Retract is 0.125

The Depth is -0.5

= 4 ‘Z’ values available in the NCI data going to the Post Processor.

 

The bolded value below is the Initial Height (which I added to the PST to get this output).

The Post variable name for it is = initht

If Clearance is ON, initht is loaded with the Clearance value.

If Clearance is OFF, initht is loaded with the Retract value.

 

G0 G90 G54 X-3. Y1.5 A0. S1000 M3

G43 H1 Z2. M8

Z1.875

G98 G81 Z-.5 R.125 F8.45

X-2.125 Y.875

X-.2525 Y-.375

G80

 

So…

With some logic added to the PST, you could handle these multiple ‘Z’ scenarios.